I'd be interested in having comments and suggestions to improve the design. The files were made with Fritzing.

Besides the schematics, you can see a picture for the first design (with two layers) then two pictures corresponding to the two layers from latest design with a smaller footprint (please note the decoupling capacitors were forgotten in first design).

I would like to have some answers about these specific points:1. When a trace must be connected to several components (e.g. ground) is it a good practice to put the solder point of one component in the path to another one rather than to create direct connections to each component ?2. What about angles ? I have avoided many right angles but is it really mandatory ?3. How close may I put a soldering hole close to the board's edge ?4. What space should I leave between a hole to tie the board with a screw and a hole for soldering ?5. May I put traces under ICs or IC sockets ?

1. When a trace must be connected to several components (e.g. ground) is it a good practice to put the solder point of one component in the path to another one rather than to create direct connections to each component ?

I understand it's important to have a star grounding scheme to avoid ground lifting but in other situations may I daisy chain components or should I avoid it too ?

Daisy chaining the ground side of lots of push buttons is OK, also for a string of LEDs it shouldn't be a problem. It's high current drawing devices and anything wired to analog input pins that really should have separate ground returns to a single 'star' point in your power distribution system.

1. When a trace must be connected to several components (e.g. ground) is it a good practice to put the solder point of one component in the path to another one rather than to create direct connections to each component ?Good Question =]

2. What about angles ? I have avoided many right angles but is it really mandatory ?Avoiding RIGHT angles is always mandatory for me, but using "45" degree angles is always good, but, not better than curve lines. But, if you search for designs, curved lines are used a lot on HIGH power circuits (so that current doesen't creates a joule effect on corners, and get hot), and in HIGH speed communication protocols, like the USB (notice on the arduino DUE, there is a "wave" made with the D+ and D-, pin where data from usb comes and goes).I use without any problem 45 degree angles (also known as "chamfer"?)

3. How close may I put a soldering hole close to the board's edge ?This depends on each company. Itead specify a minimum of 1mm (if i'm remembering well), from any hole/cooper/anything to the board edge... keep in mind, that this is something to "prevent" future problems like wear on the edges.

4. What space should I leave between a hole to tie the board with a screw and a hole for soldering ?Remember to things on this:The hole of the screw, and also the HEAD of the screw... put a margin of 2mm and everything is fine...Also, remember this: If you use a power plane on the bottom of VCC and one in the top of GND, then BE CAREFUL to remove all the cooper around the hole, so that if the screw scratches the solder mask, the screw will not "connect" the circuit with VCC and GND...

5. May I put traces under ICs or IC sockets ?Shure! just remember to follow the company guide lines (specifications). Itead needs an "8mil" minimum trace width, and 8mil minimum relief (distance from anyother thing). If, the trace can pass between two pins of the IC, and keep that minimum 8mil, it's ok =]

With experience, you'll find there is often no black and white answer to many of these questions. You have to understand something about the signals you're carrying to make educated decisions about how to treat the traces and components that carry those signals.

I just want to second some of the opinions expressed already because they bear repeating. With screw holes, print your design 1:1 and poke a hole through your mounting locations. Insert the fastening hardware you plan to use and verify the mechanical clearance to every part in proximity. I also do not recommend ever putting traces beneath the head of a screw/bolt, due to the possibility of conducting an exposed trace, or wearing through solder mask (on a produced board) and then conducting with the exposed trace. Remember to provide clearance for nuts, if the bolt head is on the mating surface and not the PCB. Remember also any tool clearance if you'll be tightening a nut with pliers, etc.

So, back to traces and such. It has long been good practice to use 45deg. angles instead of right angles. Do they have to be 45deg? No. With low-speed (say, less than 10MHz) circuits, you can get away with many sins. The higher the frequency, the more these nits need to be picked. For high-current traces (power supplies and such), gentler curves are better than sharp angles because of the thermal stresses and thus opportunity for "weak spots". Mostly, just make sure the trace is always wide enough, even when changing orientation, and you'll be OK.

In general, I strive for 100% 45deg. angles. Partly because it just looks nice, and it never hurts to develop good habits when it doesn't matter so it's second nature when it does. Of course, I'll bend the rules and use 20-70deg angles when a 45 would put a trace too close to a neighboring pin. That's almost entirely a cosmetic dispute. Furthermore, I'll try to avoid too many bends (I think of it as avoiding electrical turbulence) and too-long straight lines (subject to inductance and capacitance with things near and parallel to that trace), although I'm not sure my logic is entirely sound on either point there. It just feels like the right thing to do, and I could very well be wrong.

On proximity of holes... Always leave space around the board edge. Different fabrication houses have different requirements here, but they're almost always way more lenient than you should strive for. You don't want the board to have weak support around a component hole, so make sure not to perforate the board with too many holes in too small a space. That principle covers hole-to-hole clearance, grouping many holes too close together (Swiss-cheese style), and being too close to the edges. If it feels like you could snap a chunk out of the board, provide more solid substrate.

On proximity of traces... When two traces ride alongside each other, they will tend to couple capacitively. This is detrimental to high-frequency signals. Things that change rapidly, ala digital transitions, certainly apply as well as true HF analog waveforms. In rare cases, you can benefit from this -- like power and ground traces -- but it's better to use a capacitor when you want coupling, rather than taking advantage of the side effects of layout.

There's also inductive coupling, where the signal from one trace (or component!) can "echo" onto another trace (or component). This is usually to be avoided at all costs. Placing grounds between bleed-prone signal traces is a good approach, as is ample distance. Digital signals have (in theory) infinitely high-frequency spikes caused by low-to-high and high-to-low transitions. In reality, those transitions aren't perfect square waves, but they can still cause radiation into other signals -- especially analog. High-current traces will tend to bleed more than low-current, so keep your low and high level traces well apart from each other.

Routing between the pins of ICs, and underneath the body of components, is a common practice. As long as the trace has adequate clearance (10 mil is typical) from other traces and pads, you'll minimize the chance of shorts. Most professional fab houses can get closer, and most home etching attempts should probably be a little further. Remember of course to respect the nature of the signals on those pins. High current and high frequency signals should not be near low-level signal and analog signals. Sometimes you can't help it, so just do the best you can.

For grounding, I have a few principles I follow. The bigger the better. I'll sometimes have larger ground traces than power traces. You want your grounds to have as little impedance as possible. Strive for having every ground go back to the common ground point individually. In most cases, this is impossible to accomplish, so you have to group similar grounds and bring them back in bulk. Prioritize here. Power supply grounds should be as separate as possible from signal grounds. Analog and digital should not be shared. High frequency and low frequency will benefit from separation. Areas that are subject to crosstalk should be separate. Etc... Really try to avoid "daisy chaining" grounds from one component to another to another. Connect them to a plane instead, and bring that plane home to the supply ground. Good grounding is the art of compromise, so try to always follow best practices and bend the rules where you must. Again, prioritize.

A good thing to do is try alternate layouts. The hardest part of designing a PCB (for me) is the blank canvas, so just dive in and start working outward from there. Place your components such that they are logically grouped well. Things that attach should be near each other, and things that can disturb each other should be far apart. Rotate things and try alternate arrangements until you find a way to prevent snaking traces everywhere. Many people advise, when using two layer boards, to route traces North/South on one layer, and East/West on the other. This provides a way to keep traces from having to cross each other too much. Vias will bring top signals to bottom, and back again. But, I avoid vias as much as conveniently possible. That may or may not be necessary. In general, for less dense boards, I try to keep all my traces on one side, so I have a whole other layer to fall back on when I run out of area for grounds or power distribution, etc. There are no hard rules here, it's just a matter of what works for you and the layout demands of your project.

On v2 the top layer track between Rn and Jn seems to pass awfully close to the opposite pad on Jn...

That definitely looks too close - design-rule-check should catch this though. Personally curved tracks like thisremind me of the old days where PCB artwork was laid out by hand using strips of black crepe sticky-backedtape and a scalpel - crepe allowed the tracks to bend round without creasing.

[ I will NOT respond to personal messages, I WILL delete them, use the forum please ]

On v2 the top layer track between Rn and Jn seems to pass awfully close to the opposite pad on Jn...

That definitely looks too close - design-rule-check should catch this though. Personally curved tracks like thisremind me of the old days where PCB artwork was laid out by hand using strips of black crepe sticky-backedtape and a scalpel - crepe allowed the tracks to bend round without creasing.

Indeed, I have improved the PCB. Please see attached files.

By the way, when it comes to decoupling capacitors for ICs, can I consider this is as a special case and indeed route one pin of the capacitor to the IC's ground (as I have done in my PCB) or should I also route this pin as directly as possible to the global grounding point ?

I think it's fine to use the IC ground here. Again, use moderation with the star grounding approach. It gets unwieldy fast. Any common power elements (the IC, a neighboring IC with compatible power demands, and their decoupling caps) can absolutely share a little ground plane. Just don't run a single trace from one to the next. That invites the ground trace to raise above 0v between points, offsetting the reference level for anything in between. If you can't use a plane, use several traces that meet at a single point and trunk back to the main ground.

Here's an interesting article I just found on ground planes and how currents flow etc.

http://www.maximintegrated.com/app-notes/index.mvp/id/5450

I've not been too careful about where I run traces and it hasn't really bitten me in any noticeable way--yet--but I will be paying more attention to this particularly for analog and high frequency, neither of which I do much of; but that'll soon change I suspect.

Another thing to keep in mind (and search for articles on) are bypass capacitors and their placement and effects on noise.

As to the 45 degree bends, I am kind of OCD about that. I've seen some debates on that. Just keep in mind there are multiple viewpoints. Here's a contrarian one.

Thanks for the reference material. I often rely on general practice and gut instinct, so it's nice to see someone doing the math.

My only criticism with the author's points (re: 45 deg. corners) comes from the fact that the publication dates from 2000 (and so we are starting to see hobbyists near the frequencies of professional electronics designs at the time -- but still, not at GHz speeds), and this paragraph:

Quote

Might the electric-field concentration at a sharp, pointy corner create a lot of radiation? Hogwash. As a trace rounds a corner, it stays a constant distance from the underlying reference plane the whole way. The electric field intensity from trace to plane doesn't radically vary at any point along this track except for a modest perturbation in the vicinity of the actual pointy tip of the corner. It's true that a microscopic electric-field probe directly adjacent to the corner would detect this field concentration. However, measurements taken from farther away account for the average of everything that happens along the whole trace, not just at the corner. The corner, because it's so small, cannot noticeably affect the far-field radiation.

I could be wrong, but it sounds like this is referring to a multilayer design with a ground plane layer. I wonder how that differs from 2-layer boards with no ground plane? Also, I've heard people talk about corner radiation being an issue for compliance testing in production designs. (Also not something a hobbyist really needs to concern himself with.) Whether that's true or not, I'm not experienced enough to say.

Well, like I said ... I use a hybrid approach. It's one of those topics that'll get people from both extremes into a heated debate well over the heads of most of us. Like everything else, there are compromises to each approach, and learning where to apply one set of rules over another is something that can only be accomplished with a lot of experience, plenty of study, and a ton of real-world testing.